Calculate and Assign Midmesh Thicknesses

Calculate and assign the thickness of a midmesh from solid geometry using the Midmesh Thickness tool.

The thickness will be assigned to the midmesh either on node card, element card, nodal thickness on element card, or as properties on elements or components depending on the solver profile you are using.
Restriction: Only available in the OptiStruct, Radioss, Abaqus, LS-DYNA, PAM-CRASH 2G, or Nastran solver profiles.
From the menu bar, click Mesh > Edit > Elements > Midmesh Thickness.

Select Midmesh and Solid Inputs

The midmesh and solid can be specified by manually selecting entities from the current HyperMesh session, or by selecting external geometry or FE solver decks as input.

Figure 1. FE and Geometry with Traditional Element Visualization
Select midmesh and solid inputs.
To select input from Do this
External geometry/FE solver decks
  1. For input, choose From file.
  2. For Solid geom/mesh, choose whether to select geometry or FE (mesh), then navigate to the file that contains the input.
  3. For Midmesh, navigate to the file that contains the midmesh.
Existing entities
  1. For input, choose Select entities.
  2. Use the Solid geom/mesh selector to select input.
  3. Use the Midmesh selector to select input.

Define Thickness Output

Calculate and assign a thickness on the midmesh.

  1. Select a Thickness output.
    Output Description Solver Profile
    Nodes Assign a thickness on node cards. Abaqus
    Elements Assign a single thickness on the element card.
    • Abaqus
    • LS-DYNA
    • PAM-CRASH 2G (TSHELL and SHELL card image)
    • Radioss
    Nodal thickness on elements Assign multiple thicknesses on elements for each node.
    • LS-DYNA
    • Nastran
    • OptiStruct
    Properties on elements Create properties for groups of elements, and assign a thickness to each property.
    • Abaqus
    • Nastran
    • OptiStruct
    • Samcef
    Properties on components Create components and properties for groups of elements, assign a thickness to each property, and then assign the property to the corresponding component. The original components are duplicated, thus maintaining relevant information and attributes.
    • Abaqus
    • ANSYS
    • LS-DYNA
    • Nastran
    • OptiStruct
    • Samcef
    Select card image

    Select property/section card image

    Select property card image

    Select the card image to use for the relevant thickness assignment.

    This varies depending on the solver profile and the type of thickness output selected.

    • Abaqus
    • ANSYS
    • LS-DYNA
    • OptiStruct
    • Radioss

    Contact thickness

    Assign thickness/contact thickness on PART. PAM-CRASH 2G
    Prefix Define the prefix for generating property names.
    • Abaqus
    • ANSYS
    • LS-DYNA
    • Nastran
    • OptiStruct
    • PAM-CRASH 2G
  2. Define thickness options.
    Option Action
    Minimum thickness/Maximum thickness Define a thickness to assign calculated thicknesses.
    • To enter a minimum thickness to assign calculated thicknesses below a specified value, select the Minimum thickness checkbox.
    • To enter a maximum thickness to assign calculated thicknesses above a specified value, select the Maximum thickness checkbox.
    Assign offset to elements/sections To assign an offset value to elements if they are not in the middle of the selected geometry, select the Assign offset to elements/sections checkbox.

    Figure 2. 2D Detailed Element Representation On, No Element Offset On. The mesh deviates from the geometry; the midmesh node is equidistant from mesh corners, but not from the nodes on the geometry corners.

    Figure 3. 2D Detailed Element Representation On, Element Offset On. Offset has caused the mesh to match the geometry, though the initial midmesh node remains unchanged, such that it now matches the geometry.
    Assign average thickness to element groups To approximate the thickness values on individual elements to be an average value representing a group of elements, select the Assign average thickness to element groups checkbox.

    Only available when Thickness output is set to Elements.

    Consider a model which has a thickness variation as shown in Figure 4. If you assign thickness on elements, by default you will get a highly variable distribution.

    Figure 4.

    Each row of elements is assigned a different thickness, resulting in various thicknesses, even if the solid was captured accurately.

    Enabling Assign average thickness to element groups groups elements with similar thicknesses together, and assigns an average thickness to the groups. In Figure 5, the middle region of the model is assigned a single thickness and the right section is assigned fewer steps. The accuracy of the model captured is reduced.

    Figure 5.
    Note: This is the default behavior if the Thickness output option is set to Properties on elements or Properties on components.
    Maximum thickness range interval Control how similar thickness elements are grouped together.
    • Choose Rel (relative interval value) to specify a relative interval value, which defines the relative width of each thickness band.

      For example, suppose you enter a Rel value of 0.2. Starting from the element with the smallest thickness, elements with similar thickness are grouped together, such that the difference between maximum and minimum thickness in one group does not exceed 0.2 times the maximum thickness in the group. The thickness values of elements in a group is averaged and assigned to all of the elements in the group (or to the property.)

    • Choose Abs (absolute interval value) to specify a value to use as the cut off for the maximum range of the thickness in a group.

      If this value is 0.5, the difference between maximum and minimum of the thickness values in a group / property will be a maximum of 0.5.

      Smaller values result in a larger number of properties that will be created, allowing the thickness variation to be captured more accurately.

    Figure 6. . Assign average thickness to element groups: On / Maximum thickness range interval: Rel = 0.5.

    Figure 7. . Assign average thickness to element groups: On / Maximum thickness range interval: Rel = 0.2.
    Note: Available when Assign average thickness to element groups is enabled, or if thickness output is set to Properties on Elements or Properties on Components.
    Fixed interval with start thickness Control thickness properties at constant intervals.

    Enter a desired thickness value in the Start thickness field, and a thickness interval value in the Interval field. All elements will be grouped into properties/components with fixed increments to the thickness specified by the interval value, beginning with the start thickness value.

    Truncate thickness to range interval Round the thickness values up or down to have the same number of decimal digits as the input value in the Maximum thickness range interval field..

    There are three modes available. Automatic determines an optimal truncation.

  3. To save the information logged during the computation in a specified file, select the Save log file checkbox.
  4. Define advanced options.
    Option Action
    Correction method Select a correction method to perform on elements or nodes where the thickness could not be computed correctly.
    • Choose Interpolate from Neighbors to interpolate an appropriate thickness value from the neighboring element/node thickness.
    • Choose Adjust to min/max values to assign either minimum or maximum thickness, if they are defined, to the corrected elements.
    Scaling at corners [0,10] Enter a scaling factor to use when interpolating thickness values near t-junctions or corners.

    A value less than 1 will result in linear decrease in the thickness values nearer to the junction/corners. A value of zero will result in an approximate mass-conserved thickness estimation. When equal to 1, the thickness is extrapolated / interpolated without any scaling. When greater than 1, the thickness will increase as you go closer to the junction.

    Only available when the Correction method is set to Interpolate from Neighbors.

    Figure 8. Scaling at corners = 0, Thickness Contour Applied, Traditional Element Visualization

    Figure 9. Scaling at corners = 0, Thickness Contour Applied, 2D Detailed Element Representation

    Figure 10. Scaling at corners = 1, Thickness Contour Applied, Traditional Element Visualization

    Figure 11. Scaling at corners = 1, Thickness Contour Applied, 2D Detailed Element Representation
    Max midmesh / solid angle [0.1,90] Enter the cut-off angle in degrees.

    Enter the maximum angle (0 to 90) that the mid-mesh makes with the solid, beyond which the estimated thickness will be ignored and corrected.

    For example, the images below show the midmesh in blue, and the solid in black. In the first image the midmesh and the solid form a moderate angle. However in the second image the midmesh and the solid form a larger angle. It is possible that this area is a junction, located at the solid edge, or the solid may contain some noisy features, therefore you may want to ignore the calculated thickness and interpolate that value from surroundings.

    Figure 12.
    Max thickness gradient [0, 10]

    Measures the change in adjacent thickness values, and restricts the gradient.

    Enter the maximum change in thickness allowed across two adjacent measurement locations, as a factor of the distance between the locations. Allowable factors range from 0 to 10.

    For example, the image below shows a tiny projected boss in an otherwise planar area, which you may want to ignore. Defining the Max thickness gradient specifies the cut-off for the ratio of difference in thickness at two locations to the distance between the two locations. If the ratio is more than the given value, the measured thickness is discarded, and interpolated from its neighbors.

    Figure 13.
    Max relative faceting error Enter a maximum relative faceting error to use during faceting calculations.

    When HyperMesh computes the proximity with a solid, it does not actually compute with the surface geometry. Instead, HyperMesh computes with the tessellated approximation (facets) of the geometry. In case of curved geometry, the facets may not exactly match the geometry, and hence the thickness is computed, causing faceting errors. Specifying the Max relative faceting error enables you to control the accuracy of the tessellation used, as a factor of the estimated thickness. The Max relative faceting error is the ratio of the maximum error of facets to the estimated thickness. If it exceeds this value, facets are further refined to better capture the geometry.

    Max search distance Enter the maximum distance which will be considered for searching solid proximity. This value is also used to restrict the maximum distance from which a good thickness value is considered for correcting an incorrect thickness estimate. You can also used this option to restrict the algorithm from assigning incorrect thicknesses for the mid-mesh that is out of the solid proximity.
    Do not assign thickness to midmesh outside solid Do not assign a thickness to the midmesh outside of the solid.
  5. Click Calculate Thickness.
The thickness is computed and assigned on the midmesh.

Define Visualization Settings

Define visualization settings for the midmesh.

Define visualization settings for the midmesh.
Option Action
Element coloring by thickness Set the Element Color mode to By Thickness resulting in a contour plot of thickness.

Figure 14. Thickness Contour Applied, 2D Detailed Element Representation
2D detailed element representation Display midmesh elements as 2D with the assigned thickness as depth.

Figure 15. 2D Detailed Element Representation
Assigning a thickness for each individual node or element, enables you to assign a variable thickness to elements. You can visualize both the element and nodal thickness in the graphics area by selecting 2D Detailed Element Representation from the Visualization toolbar.
The behavior of 2D Detailed Element Representation depends on what you assigned a thickness to. For example, if you assign a component an element thickness, then the element thickness representation will be displayed. If you assign a nodal thickness to an element node, then each individual node thickness will be plotted and you will be able to see the first and second order trias and quad elements. When you assign a nodal thickness, you can select the By Thickness option in the Visualization toolbar to display each node value. If you assign a nodal thickness, and offset is on, then the element thickness from the nodes will be calculated, the element will be offset, and the nodal thickness 2D Detailed Element representation on the offset elements will be plotted.
Restriction: Composites with variable thickness are not added for this feature.
Highlight corrected elements Highlight the elements whereby the thickness could not be calculated from solid, and deploy the correction method.

Figure 16. 2D Detailed Element Representation, Corrected Elements Highlighted